Help to solve the challenge of hexhedral meshing of inner edges with fillet.

[19251758]

Without fillet as in the high stress edges in defected pipeline above, the accuracy of the simulation is low. On adding fillet to mitigate the high stress edges/ sigularuty effect I struggle to get a hexahedral mesh, please I need the steps to achieve that.

Kind regards

Martin

[peteroznewman]

In SpaceClaim, split the body into solids that are easily hex meshed and a solid that has the fillet.  On the Workbench tab, use the Share button to keep the mesh connected across the bodies by sharing nodes on the split faces.  In Mechanical, right click on the bodies to be hex meshed and mesh those first.  Mesh the fillet body last with tet elements.

[19251758]

Thank you kindly Peter for the modeling suggestion. With the 5mm fillet, I have 1/4 defected pipe divided into sweepable parts. I do not know why I am still having error messages in trying to hexa mesh this. Please I still need your help.

 

Kind regards

Martin

 

[peteroznewman]

Upload your .scdoc file to a file sharing site and reply with the link.  If using Google Drive, make sure to Share so that Anyone with the Link can download it and not leave it at the default Restricted share setting which means no one with the Link can download it without first getting permission from you.

[19251758]

https://drive.google.com/file/d/1o8RwyJa7Ill1Da0T_qcmtkUjlELuxa27/view?usp=sharing

[19251758]

Good morning Peter,

Please find the link to the quarter pipe in Ansys spaceclaim above.

Kind regards

Martin

[peteroznewman]

I don’t have access to 2024 R1, so I have meshed this in 2025 R1.  Notice how I have used parallel planes 5 mm on either side of the fillet.

A finer mesh can be put on the fillet, by using twice as many elements through the thickness of the rest of the body.

To put a finer mesh on the fillet add face sizing to the fillet. Selective order of meshing can sometimes create more hex elements on the extruded shape.

Adding a Hex Dominant Method to the fillet block.

[19251758]

Good morning Peter,

Thank you kindly for solving this problem that has been a challenge, I will carefully follow the steps you explained and try to achieve the same result. But please could you save the file in a lower version (2024 R1) and share the link.

Kind regards

Martin

 

[19251758]

Otherwise I can download the student version of 2025 R1.

Kind regards

[19251758]

Good afternoon Peter,

I have done some meshing but still trying to improve the accuracy, please see below. When I applied refinment at the fillet, the removes the entire hex mesh.

Kind regards

[peteroznewman]

Hello Martin,

Ansys can’t save projects as older versions of the program. Here is a link to the Ansys 2025 R1 archive. https://jumpshare.com/v/CoTzIWqIgxwkPIYAr4Mx

You will see that I use Edge Sizing mesh controls to force the mesh to stay aligned by choosing the Hard option and selecting all the edges that I want to stay aligned. 

Though more hex elements are created at the surface using the Hex Dominant method on the fillet corner solid, there are some skinny elements below the surface that allow hex elements at the surface.

Regards,
Peter

[19251758]

Good afternoon Sir,

Please I have been working on this particular model to improve the mesh element quality yet it appears the meshing has not improved whenever I check in the mesh metric, please I need some help.

 

[19251758]

Good afternoon Sir,

After splitting the interacting defected pipeline, most of the solid parts were sweepable apart from 2 parts.

I do not understand why I am getting poor quality mesh. Please find the pipe attached here-in. 

https://drive.google.com/file/d/148jbore67vbSY1mCLOLdwUfgiDDe7I7Y/view?usp=sharing

https://drive.google.com/file/d/148jbore67vbSY1mCLOLdwUfgiDDe7I7Y/view?usp=sharing

Kind regards

Martin

[peteroznewman]

Hello Martin,

You should show where the poor quality elements are using the Mesh Metric function.

A plane used to split the solid created sliver faces which can lead to poor element quality.

Some mitigation can be done in Mechanical by inserting Virtual Topology to merge those faces, however, VT caused the gray body that was originally sweepable to become not sweepable.

I recommend you go back to SpaceClaim and more carefully create planes to split the solid such that no sliver faces are created. After I Combined some solids into one body and used a more precise horizontal split plane, when I tried to reuse a vertical split plane, new inaccurate faces were created as can be seen in the image below.

My suggestion is that you locate the split plane a short distance away from a blend edge. Don’t locate a split plane coincident with a blend edge.

[19251758]

Good afternoon Sir,

Thank you kindly for all your response, I am grateful. I have placed the split plane away from the blend edges as adviced, please find the link attached here in.13 sweepable bodies out of 15 solid parts were confirmed. At the Ansys mechanical, after setting the symmetric region, I right clicked on mesh, pressed the mesh start record button and started generating hex mesh for all the sweepable parts, element size for areas away from the defect were made coarse. At the defect area, I made use of edge sizing to achieve the needed element size.

I am still having issues with my meshing, please can I get your advise on the steps to complete the meshing with good element quality. The meshing I did, the element quality was poor, mostly less than 0.2.

Kind regards

Martin                                                       

https://drive.google.com/file/d/1G6-FhNpD8qZCoEZHOQe7FBfvU_aau0gt/view?usp=sharing

 

[19251758]

I received the following warning;

Some of the elements on the problematic bodies can't meet the specified target metrics. Please check the elements and try changing the mesh size settings to achieve the needed mesh quality.

The surface mesh is intersecting or close to intersecting, making it difficult to create a volume mesh. Please adjust the mesh size or adjust the geometry to fix the problem.

Kind regards

Martin

[peteroznewman]

Hello Martin,

I am using Ansys 2025 R2 so you may or may not see exactly the same in Ansys 2024 R1.  Below is what I see in Mechanical when I open the Aug-04-2025.scdoc file.

Notice that the Show Vertices and Close Vertices are turned on in the Display ribbon.

The close vertices are highlighted in yellow.  This is feedback to you that the geometry is not clean.  You should not have any close vertices. However, the mesher is often clever enough to ignore them.

In Ansys 2025 R2, there is a Mesh Quality Worksheet. I wouldn’t pay attention to the red bar with the Minimum Element Edge Length.  That is not the cause of any poor element quality.
The warning limit for Max Skewness is 0.9 and this mesh has a Max value of 0.99892.  Elements over 0.9 are highlighted here:

Zooming in you can see that the tet elements in the corner are the problem.

You have a 5 mm setback from the blend to the plane to slice out the sweepable part.  If you increase that to 15 mm, you might leave sufficient space to allow the elements to mesh with better quality.

A good approach here would be to use just 2 planes to cut the slot out for Tet meshing with an element size of 4.5 mm on that solid, while the other three hex meshed solids have a Body sizing of 9 mm. These values ensure that 2 quadratic elements are across every section of the model, which is the minimum recommended number.  Bonded contact keeps the two cut faces on the slot solid bonded to the other two solids.

In SpaceClaim, hide the slot solid and use the Share button to keep the mesh connected on the three bodies with the Hex mesh so you don't need Bonded contact on those faces.

[19251758]

Good afternoon Sir,

Thank you kindly as always for your assistance in my modeling. Please sir, I wanted to use the last approach to model the defected pipe attached below, here hexahedral is used for the meshing of the entire corroded pipe. Tetrahedral only used for rigid body meshing. 3 layers of elements at the defect region and 6 layers at the space between defects( this is a quarter of interacting defects)(width and length of mesh at these area of interest 2mm). Please I need your help,I have not gotten the right failure pressure reflected in the journal, I think I need to get my mesh accurate first.

https://drive.google.com/file/d/1Z3t4hL94VcEwTI2oKZeBv2RdWGH9Riud/view?usp=sharinghttps://drive.google.com/file/d/1Z3t4hL94VcEwTI2oKZeBv2RdWGH9Riud/view?usp=sharing

 

Kind regards

[19251758]

Sir,

This is the updated drawing, length of defect is 300mm.

https://drive.google.com/file/d/1_q48Vjb7UAMzoYYfr3wKUvbhxBTInCIw/view?usp=sharing

 

[19251758]

This is what I generated after meshing.

[peteroznewman]

Now that there are no fillets, every face can be used to divide the solid into six sided solids.

For example the cap on the end should be split using the inside cylinder.

With no mesh controls other than setting the Mesh details as shown below.

I expect with some Edge Sizing to with the Behavior set to Hard, I could get 3 elements across the thin section.

[19251758]

Good afternoon Sir,

Thank you kindly for your prompt response.

In this model, my aim here is to model interacting correded pipe subjected to internal pressure and axial compressive stress.

The mesh below has 34836 elements and 164338 nodes but element display shows

[19251758]

In applying the combined loads, under analysis setting, I used 2 number of steps, step 1 - axial compressive stress only, step 2 - introduction of internal pressure plus axial compressive stress. The degree of freedom is applied as below in yellow,constraine in x and y direction, the pipe material is mild steel, but the end cap is made of rigid body material- for even distribution of axial stress

the modeling failed with some messages"There could be possible overconstraint between the bonded contacts which use the MPC formulation, to identify those overconstraint regions use the Contact Trackers or the Status under the Contact Tool".

I don't know if the DOF, mesh or axial stress that caused the buckling

Sir please would like to know your advice

Kind regards

[peteroznewman]

Since the buckling occurred in Step 1, it is due to the compressive axial load.  You should plot the graph of total deformation versus time to see at what value the graph suddenly goes up.  You should plot the last converged increment of load so you can easily calculate the last axial load value by multiplying the time value by the load magnitude.

When you say “end cap is made of rigid body material” do you mean under the Details for that solid, the Stiffness Behavior is set to Rigid, or do you mean that the material assigned has a much higher Young’s Modulus than mild steel but the Stiffness Behavior remains as Flexible?

Why introduce an artificial condition on the end-cap in the model? If the real end-cap is not rigid, making it so can alter the onset of buckling.

If you used the Share button in SpaceClaim, there is no need for any Bonded Contact.  Is there in fact any Bonded Contact under the Connections folder?

What DOF constraint did you apply to the bottom side of the model?  A point constraint is unrealistic.  What are the real supports for this structure?

[19251758]

Good morning Sir,

The main pipe body has young modulus of 200GPa, the end cap which is the rigid body section,20mm thick has higher young modulus of 200000GPa, which is to allow for equal distribution of axial compressive stress.

At the bottom side of the pipe(yellow) DOF was applied using displacement, constrained in the x and y to prevent unwanted rigid body movement, but z direction allowed movement.

[19251758]

I made use of the shared button in the spaceclaim, model attached here in.

https://drive.google.com/file/d/1QjxxIcfibKXPlFdOQhhcXoC3OkdfPcng/view?usp=sharing

when the defected pipe is subjected to combination of axial compressive stress from the outer end cap and internal pressure, one can then predict failure pressure of the pipe, when ultimate tensile stress equals von mises equivalent stress.

[19251758]

the successful modeling of the pipe failure pressure may look like the diagram below, I have not found out how to get that

[19251758]

kind regards

[peteroznewman]

Displacement is a symmetry BC. The same geometry appears on the opposite side of this plane.

Displacement 2 is a symmetry BC.  This means that if you reflect the model about this plane, you will get the same geometry on both sides of the plane.
How is it possible that you have the same defect in wall thickness on both sides of that plane with a narrow band of full wall thickness at the center?
It seems it would be more correct to slice the pipe half way along the length of the defect on the red line and apply the symmetry there. Do you agree?

Displacement 3 is a single vertex that prevents the rigid body motion along the Y axis.

An alternative model would be to extend the pipe the same distance in the +Z direction and put an end cap on that end also.

[19251758]

Good morning Sir,

Thank you kindly for your prompt reply. The longitudinally aligned interacting defects are in both sides of the plane, the symmetrical quarter pipe is made up of 300mm length defect and the narrow band of full wall thickness at the centre is (13.69mm long), but has the full defect space between the two alinged defects as(13.69x2 - 27.35mm long), hence the quarter pipe seems correct to me.

My task is to follow the modeling procedure of this journal paper attached here in, try reproducing it before introducing my own modifications.

https://drive.google.com/file/d/1L27wd3uBhSzW7GHmTWtVLtDFZVzqo6OJ/view?usp=sharing

Kind regards

[peteroznewman]

Thank you for the paper. Now that I have read that, I understand the symmetry condition you applied correctly simulates two longitudinal defects.

This image from one of your models

suggests that the boundary conditions are not correct. I can check what you have. In Workbench, use File, Archive to create a .wbpz file and upload that to your Google drive and reply with a link.

[19251758]

Good morning Sir,

Please find attached here in the wbpz file. I attempted shifting the position of the DOF to be on the 20mm rigid body side, the buckling was not there again, but it is not yet correct.

https://drive.google.com/file/d/1nmy6-i6XzsqS5PZQI7g12FAynh5u-G4U/view?usp=sharing

[peteroznewman]

Looking at the Engineering Data, you have defined a Bilinear Isotropic Hardening plasticity model with a 360 MPa yield strength and a Tangent Modulus of 14500 MPa.  The paper uses a Multilinear Hardening curve.  You would get results closer to the paper if you digitized the true stress-strain curve and put it in that material model.

Looking at the no defect model I see a few problems.

1. There is only one element through the thickness. You should change the mesh method to Sweep and select the inside face as Source so you can specify 3 elements through the thickness.
2. At one end, you have a fixed support, at the other end, you have a symmetry condition. When the internal pressure load is applied, the Poisson's ratio causes an axial tensile stress in the pipe wall. Is that your intention?
3. 
4. If I delete the Fixed Support and add a Y=0 constraint on one vertex, I get a very low state of axial stress. 
5. 
6. You should add a Cylindrical Coordinate System at the center of the pipe.
7. 
8. The material has exceeded the yield stress and entered the plastic strain region of the material model.
9. 

Looking at the axial stress + internal pressure model I see a few problems.

1. There is no need to use an element face for the DOF-1 Displacement support.  It doesn't survive remeshing. It is better to select a vertex.
2. 
3. The internal area of the end cap is 30788 mm^2, the pressure in step 2 is 24 MPa.  That creates an axial tensile force of 7.39e+5 N but the Remote Force on the end cap only applies 6.56e+5 N therefore the net axial force is tensile, not compressive! If you suppress the Symmetry region for the Z direction and put a Displacement of Z = 0 boundary condition on those faces, you will find the Force Reaction at the end of step 2 is a slight tensile load of 0.88e+5 N or the difference between those two loads. Is this what you intended?
4. In Ansys 2025 R2, the the PCG iterative solver is automatically selected by Program Control logic and solves in about 9 minutes on my laptop, but the Direct solver takes 8 minutes to solve.  I changed from Program Controlled to Direct.

[19251758]

Good afternoon Sir,

In this modeling, I want to find the failure pressure( when the equivalent stress Von mises will be equal to the true ultimate tensile strength) of the defected pipeline.

I have removed the DOF from point constraints at the symmetry face(as you advised) and placed it at the OD, outer diameter of the rigid circle. I made use of the name selection for this outer cylinderical surface of rigid ring, then inserted the displacement; ux=0,uy=0, uz=free (free axial movement).

I also left the rigid ring out, when scooping the inner pipe for internal pressure and for the equivalent stress-von mises plotting.

I have focused the remote force only on the (outer) annular face of the rigid ring. Please I will be attaching the current file for you to see and comment. The DOF error on the journal had made it very difficult for me to compare results with the journal.

[19251758]

https://drive.google.com/file/d/1nmK8NI8PtM8sjjDloBPxdNsXNQz3RO0F/view?usp=sharing

[19251758]

Good morning Sir,

Please find attached here in my updated modeling for axial stress and internal pressure, I have made additional corrections, yet the model has not converged.

https://drive.google.com/file/d/1StfVs2oIkXQn3Zvp0niG0t3W1FE70_Ua/view?usp=sharing

[peteroznewman]

You misunderstand how to identify the burst pressure in a nonlinear plasticity material model.

You do not want the model to converge. Ideally, you have a model that fails to converge after an exponential growth in displacement as the pressure is applied gradually.

If you plot Pressure versus Maximum Total Deformation, you get exactly that. I have made a chart of that below.  This is one way to define burst pressure.

You must ignore the unconverged row in the Tabular data. The last converged row has a pressure of 18.321 MPa, which is the failure limit.

The paper you provided used a different definition of failure.

[19251758]

Good morning Sir,

What I mean is that I am still trying to generate a clean result, I realised that the failure pressure is about 18.321 MPa. Something is still preventing me from getting a clean completed result.

Kind regards

[peteroznewman]

What do you mean by a clean completed result?  Do you mean that the last load increment did not converge and created the messy unconverged plot at time step 2? If you want the analysis to end just before it does not converge, simply put in a pressure load of 18.3 MPa. However, that is unnecessary because you already have that result. It is the second last result in the tabulated data. What is preventing you from using that result?

Here is a video I made: https://www.youtube.com/watch?v=qMmEhZll0kI

You could choose to use the same definition of burst pressure as the paper used instead of the definition I explained above.  From the paper:

[19251758]

Good afternoon Peter,

Thank you kindly for all your time to answer my questions. The video was helpful and you have already explained the issue I was asking. I was bent on getting the results as it was in the Journal paper.

Kind regards

Martin